CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Mass conservation in multiphase problem (http://www.cfd-online.com/Forums/fluent/74489-mass-conservation-multiphase-problem.html)

cna April 1, 2010 09:37

Mass conservation in multiphase problem
 
Hi all,

I am working on a two-phase flow in a hydrocyclone using the eulerian multiphase model. A mixture air/water is entering at 4m/s the hydrocyclone of a dimension of approximately 1m high. Even when the solution seems to be stable, only approximately 2kg/s on a total of 4kg/s are leaving by the outlets. I tried to decrease the limit of the residues from 0.001 to 0.0001, to increase the discretization orders (momentum and turbulent quantities from 1st to scd order) but this deficit in mass doesn't change a lot.
I used the k-e RNG Swirl dominated flow and the Quick volume fraction discretization.
In the boundary conditions I retain the default turbulence specification method (k-e) instead of the Intensity and Hydraulic diameter and I worked with the 3d version and not the 3ddp.I don't know if these parameters can explain my lack of mass conservation...?
Is there someone having an idea for my problem?
Thanks a lot

thecfduser April 1, 2010 18:15

Hi
1-Why are u enetring air in a hydroclone??
2-how are u choosing ure dispersed phase dimension????

For ure mass conservation problem:
1- are u using steady or unsteady solver????
2- did u monitor any data ????
3-3d or 3ddp will give u the same results.
4-u are not using QUICK for quantities other than volume fraction??

cna April 2, 2010 08:42

The device is a separator (Stairmand), sorry.
I took 1mm of diameter for the water dropplets but without any specific reason.

I am using the unsteady solver.
I monitored the volume fraction and I could see from the distribution of the volume fraction that it didn't change a lot at the end of the simulation (during 8 secondes on a total of 15 secondes), as it is for the mass imbalance.
I used Quick only for the volume fraction.

Thank you for your answers

thecfduser April 2, 2010 14:45

Hi
are u monitoring mass at the outlet ????
I mean that if u look to the mass at the outlet, it will not be the same as at the inlet because u are using unsteady solver, so u can allow accumulation. But as u say, in average it will be the same. I dont know if ure problem is here...
Anyway, i advice u to use QUICK for all quantities as in a highly swirling flow, a high order discretisation is very important.
Ure time step is how much??? do u have problems with turbulent viscosity ?

cna April 3, 2010 08:30

At what it seems to me the end of the simulation I have checked the report fluxes for the mass several times and so I can see that the mass at the outlet doesn't change significantly in order to balance the inlet flux.
In the beginning my time step was of 0,0005s but in the end I could increase it to 0,01 without divergence, I think because the solution was nearly steady-state.
I had some convergence problems when I tried to use second order discretization but not with the 1st order discretization (for momentum and turbulent quantities).

thecfduser April 3, 2010 18:56

Hi
in fact, as ure flow is unsteady, ure flow at the outlet will never be the same at the inlet. Are u sure that the inlet flow was always superior to ure outlet flow??? try to monitor it to be sure. Remember that in cyclones, u often have a reversed flow (a reversed core) that can extend to the outlet, so most of the time, u can have a small outlet flow, that abruptly get bigger for short moments...
As u say, with second order discretization u can get convergence problem. the way to avoid this is to refine time step. 0,0005 is very good . 0.01 is too big: even if u dont diverge (specially that u are using an implicit time stepping) ure solution of course will not be good. according to my experience, ure velocities can very enormous......
My advices: use QUIck, use a fixed time step. Verify that ure mesh is enough small. A very large mesh (specially with distorsed elements) or a non conformal grid, all this can cause big mass imbalance.
( 1 iteration by time step is sufficiant, but keep ure time step<0,0005)

If u have any of these problems, tell me and i can give more help

cna April 4, 2010 10:16

Thank you very much for all your advices, I will apply them!


All times are GMT -4. The time now is 04:56.